Sub-Assembly and BOMs

Our corporate drafting standard will not allow bills of material on
our drawings. The numbering of balloons on an assembly drawing must
match the item numbers of the corresponding BOM gernerated by our MRP
system. While this is a pain in the butt, we work around this by
carefully managing the order of the parts in the FeatureManager.

I'm now working on some very large assemblies. I'd like to break a
large assembly into smaller sub-assemblies to simplify the modelling
process. My problem is that these sub-assemblies will not be entered
into our MRP system, and thus will not show up on the master bill of
materials. I need to be able to have an individual item balloon for
each component of the sub-assy.

I know that I can select "Show Parts Only" in the BOM Properties
dialoge box, but this give an individual item number to every single
part. (The indented bom doesn't help me 'cause there won't be a bom
drawing) Some of the sub-assemblies are models of off-the-shelf
products, so the entire sub-assembly should be identified by one
balloon number. Some of the assemblies are weldments. Again I don't
want each piece of the weldment to have a balloon number, just the
finished weldment.

Is there away to have some sub-assy identified with one item balloon,
while applying individual balloons to each component of other
sub-assemblies?

(I hope this makes sense. It's been a long day!)

Thanks for the help

Rob

 

New Corporate Standard.

 

Actually maybe you could do an indented bill and uncheck the sub-assemblys
you don't want in there. I think you may end up with gaps in your numbering
scheme though. I have heard 2004 handles BOMs a bit better but will it
solve your problem someone else may know.

 

Sounds like your MRP people, do not understand drawings.

Isn't the Bal Ref just a field in the MRP system under the Assembly number?
Also, how do you handle the same part used on a different Assembly where the
Bal Ref would be different?

 

Rob,

You've stumbled across the age old problem of engineering BOM vs.
manufacturing BOM. Engineering BOM's are geometric specific while
manufacturing are item master specific.

As a designer I am concerned with correctly representing the geometry
in a model. As a purchaser, all I'm concerned with is how many parts I
have to buy and when in order to meet my MRP requirements for
production builds. Hence your current problem.

The easiest solutions is to look at the various workgroup PDM systems
that are relatively inexpensive and very powerful.

For example, I am using DBWorks (Solidwork's Gold Partner)to generate
an engineering BOM. DBWorks allows you to designate sub-assemblies as
a single part (As it would be if you were given a supplier model but
purchased the assembly as a single line item on your purchase order).

Advantages of DBWorks (as applied to BOM's) include:
- Can designate parts as make, buy, or no BOM (the latter is what you
want to designate all the sub-components that make up the purchased
assembly).
- Can add phantom parts with quantities (including A/R)without needing
any SW models (i.e. Blue Loctite - 6 drops, part number XXXXXX).
- Can format the engineering BOM (Excel template) to create a format
specific file that your MRP system can batch input (rid yourself of
the dual entry dilema when converting engineering BOM to manufacturing
BOM.
- I havent' tested this but you may be able to assign a balloon (item
or find number) to each part which would match your MRP find number.
You may be able to have a script file modified which checks the type
of BOM in DBWorks and assigns that data field to your drawing balloon
callout. This would be a project specific value which would allow you
to have different numbers for your various projects.DBWorks, like SW
has a open API that allows you to create just about any solution you
may require.

Additional benefits of using these workgroup PDM's include automatic
filling out of drawing titleblock values (batch mode); Revision
control of model and drawing files (including configurations);
Approval control; Product definitions, elimination of the "he/she who
saves last wins" game in a multi-seat environement, etc.. etc..
etc.... Powerful stuff for an 800.00 USD program.
I need to confirm this but I was just told it allows multiple
materials in a single part model. How about a single Toolbox part file
that contains a carbon steel, 18-8 SST, or nylon (.250-20 X 1.00 long
3A UNC) bolt that correctly configures itself (density, cross section,
material call-out) in drawings and models?


Hope this has helped.

Len K. Mar, P.Eng.
President
E-data Solutions

 

G'Day Tony!

Yes, I don't believe that our MRP people understand drawings.

To answer your questions, yes the balloon ref is a field in the MRP
system. You look at the balloon number on the drawing, find the
corresponding ref on the MRP bom and that gives you the part number.
A part used on two assemblies can have different balloon numbers, but
the part number will be the same.

Rob

 

Why not just use "Custom" instead of "Item Number"? Then you get to keep the

We could do that. Its just much more labour intensive. Besides I'm
sure that I'd screw up the numbering.

I was hoping that SW would allow me to expand the BOM the way I could
with MDT and Inventor. With those programs, you open the bom dialoge
box and a plus sign would be beside each sub-assy in the bom (much
like a folder with sub-folders in Windows Explorer). Just click on
the plus sign, the bom expands showing the sub-assy's components, and
item numbers (balloon #) are assigned to the components. The sub-assy
is then greyed out. To collapse, just click the minus sign.

One of the very few things I miss about MDT.

Rob

 

ROTFLMAO
I'm a new user of SW
and are going through the same
crap. Our system has been in place before
semi affordable CAD even existed (Drafting table days)
And it's very difficult to even suggest
a change in drafting/documentation standards.
In other words I have to make SW adapt
to our system ..... Period!!!!!!!!!!!!!!!
No if and or butts

 

I guess I should have used a smiley face or something I meant it more as a
joke. I understand that in many companies this would be an imposibility.

Corey

 

One way you may be able to separate your subs that are Weldments and Subs
that are not is to save your Weldments as Part files this way you would have
2 models of your weldments one as an assembly one as a part. Then you
insert the part one into your top level assembl as a single part. The only
problem you may experience is when changes are made to the weldment it will
not be associative and to update the part file you will have to save over
it. I don't know what this will do to your top level. Your mates may go
hay-wire but I haven't tested it. The only other thing I could suggest is
get someone to build an API that would do what you want.

Regards
Corey

 

Don't worry Corey, It's a joke indeed.
That's why I'm laughing and crying in my beer

 

No use crying over spilled milk. :^)

 

Rob,

PDM/Works will not do what you want unless you spend considerable
money creating a custom program. In order to gain access to the
PDM\Works API you will have to shell out $5K to get the advanced
server plus x dollars for the customization (which will need to
include a DB in order to be able to tag the different balloon numbers
in different assemblies).

I've tried to make PDM/Works do what I want for the last 4 years
without success. DBWorks is $200.00 cheaper and 10x more powerful.
You'll want them to show you exactly how it will do what you've asked
in previous posts. I've beta tested PDM/Works 2004 and cannot see any
new functionality that would allow you to do this. I'd skip the VAR
and go directly to SW customer support or product manager.

I'm going to go out on a limb here and guess your VAR will try and
steer you to Smarteam in order to get this "functionality".

Email me if you want any more detailed information. We can take it
off-line.

Cheers,

Len K. Mar, P.Eng.
President
E-data Solutions

 

Have you tried using the option to not show child components in BOM
when used as a sub assembly. It is in the configuration properties.
You can turn it on for any subassemblies that you want to be numbered
as a single component and off for the subs that you need to see the
parts of. Then you can still use the BOM option to Show Parts Only.

Todd

 

Thank you Todd!

I was carefully watching this thread since this is also a problem I had. I'd
never seen this little option before. I don't know if it will help Rob but
it will definetely help me with those sub-assemblies I wish to treat as a
single item in the BOM.

You made my day, have a nice one!

Pascal

 

Weldments aren't really assemblies, a finished weldment is really a
part. The way we handle that is creating an assembly showing all the
pieces of plate etc. then use "Join" to turn that into one part which
represents the finished weldment. That part is what's inserted in the
next level assembly. Perhaps you could apply this same idea to
purchased assemblies too? At any rate this suggestion might solve part
of your problem. The only real downside to it is changes to the
weldment assembly don't update automatically, you need to open the
join.sldprt to propogate the changes.

Your product structure should match your feature manager. I don't
agree with creating subassemblies for ease of modelling an assembly
when that means your feature manager items don't jive with your MRP
BOM. Maybe you should keep everything as individual parts and try to
use folders instead to organize things.

It's not just an organizational matter either. You end up with
assemblies that don't have associated part numbers or drawings. Just a
bunch of orphan assemblies created out of short term convenience.

 

Devlin quipped:

while i agree with you, this is exactly counter to what SW and my VAR have
said: With large assy's, use sub-assy's to make the large assy easier to
work with.

The big problem is that your SW BOM will NEVER match your MRP BOM.

What I really want is an option something along the lines of: Make all
components of this sub-assy appear as top level in the big assy.

ie: I have a forming slide assembly, and a wire puller slide as sub-assys in
my main assembly. Neither one is an assy as far as MRP is conerned tho.
Now, I have a plate that is used in both sub-assy's #P-6495-3. My MRP BOM
shows a quantity of (2) #P-6495-3. There is no way to see (2) of those
parts in a SW BOM. The option above would remove the two slide assembiles
as far as the BOM is concerned, and it would show (2) of those plates.

you can't tell SW to show parts only, since it will "dissove" all the
sub-assy's WITHIN the slide assy's. Since I have MRP-assy's within each
slide SW-assembly.

I'm sure the folders help (well, i know they do) as far as organization
goes, but they don't help as much as far as performance goes, since the
point of creating sub-assys for SW is to help performance. And keep
mategroup1 to a reasonable level. The fewer mates to solve in the main
assy, the better off you are. SW doesn't need to resolve the mates within
the two slide assemblies each rebuild, but would need to if all components
are inserted to jive with the MRP BOM.

--nick e.

 

GREAT!!!!

Thanks Todd, that is exactly what I was looking for!

It's going to be a bit of a pain in the butt going back and turning
this on for all of the sub-assemblies I don't want expanded in the
bom. SW should have option turned on by default.

Thanks again!

Rob